CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

InterFoam fails to predict suspended stationary liquid column in capillary channel

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   April 11, 2014, 16:14
Default InterFoam fails to predict suspended stationary liquid column in capillary channel
  #1
Member
 
Ovie Doro
Join Date: Jul 2009
Posts: 99
Rep Power: 10
ovie is on a distinguished road
Hi:

I have a set up where a slug of liquid (water) is suspended in a vertical capillary channel open to the atmosphere at both ends. Experimental results from our lab shows that the liquid is unable to flow under its weight without agitating the channel. However, when I run simulations using interFoam for the set up, the liquid easily flows under the influence of gravity (see attached file for 2D case).

I guess the question is should the no-slip boundary condition be used in this case or should it be replaced by some friction dependent bc that accounts for the effect of a static friction barrier that must be overcome before liquid starts flowing?

Thanks.
Attached Files
File Type: zip capillaryStationaryLiquid.zip (8.8 KB, 40 views)
ovie is offline   Reply With Quote

Old   April 13, 2014, 17:15
Default
  #2
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,020
Blog Entries: 39
Rep Power: 109
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
Greetings Ovie,

I haven't managed to look into this, but I'm still curious... I'm making a note to come back to this in a few days.

Anyway, my guess is that you did not initialize properly the pressure field. The other possibilities that come to mind are:
  • Mesh isn't good enough.
  • The dimensions of the tube might be incorrect.
  • The alpha contact angle algorithm should be able to handle this. Did you follow the same steps as in the "capillaryTube" tutorial case?
By the way, you might want to try and initially run the simulation without gravity or with the vector perpendicular to the tube wall, for a few seconds. Then after the simulation stops, change the gravity vector and then continue the simulation from the last time snapshot.


Best regards,
Bruno
__________________
wyldckat is offline   Reply With Quote

Old   April 13, 2014, 20:39
Default
  #3
Member
 
Ovie Doro
Join Date: Jul 2009
Posts: 99
Rep Power: 10
ovie is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
Greetings Ovie,

I haven't managed to look into this, but I'm still curious... I'm making a note to come back to this in a few days.

Anyway, my guess is that you did not initialize properly the pressure field. The other possibilities that come to mind are:
  • Mesh isn't good enough.
  • The dimensions of the tube might be incorrect.
  • The alpha contact angle algorithm should be able to handle this. Did you follow the same steps as in the "capillaryTube" tutorial case?
By the way, you might want to try and initially run the simulation without gravity or with the vector perpendicular to the tube wall, for a few seconds. Then after the simulation stops, change the gravity vector and then continue the simulation from the last time snapshot.


Best regards,
Bruno
Hi Bruno: thanks for your feedback.

The set up for the 2-D version of this problem is adapted directly from the "Capillary Rise" tutorial - so i used the same set of the initial conditions. I also retained the same mesh resolution as was used in the tutorial. The dimensions have been double checked and they are ok too.

The suggestion to turn off gravity at first sounds good. I would try this out and let you know the outcome.

Thanks again!
ovie is offline   Reply With Quote

Old   April 14, 2014, 15:25
Default
  #4
Member
 
Ovie Doro
Join Date: Jul 2009
Posts: 99
Rep Power: 10
ovie is on a distinguished road
Quote:
Originally Posted by ovie View Post
Hi Bruno: thanks for your feedback.

The set up for the 2-D version of this problem is adapted directly from the "Capillary Rise" tutorial - so i used the same set of the initial conditions. I also retained the same mesh resolution as was used in the tutorial. The dimensions have been double checked and they are ok too.

The suggestion to turn off gravity at first sounds good. I would try this out and let you know the outcome.

Thanks again!

Hi:

I just repeated the simulations with/without gravity. The case with gravity was ok i.e. liquid remains suspended in capillary channel. I ran this for enough time to ensure the solution is stable. Then I restarted with gravity turned on and the liquid slug starts flowing downwards. The liquid slug has a volume of 5microL and the channel volume is 70microL. The velocities from the interFoam solution approach values from Poiseuille flow which is really high for channels of this dimension. I dont think these results are correct.

Thanks.
ovie is offline   Reply With Quote

Old   April 14, 2014, 16:00
Default
  #5
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,020
Blog Entries: 39
Rep Power: 109
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
Hi Ovie,

Mmm... I think you might be hitting the limitation mentioned on these posts:
Last but not least, as mentioned on the post #15 on the last thread, you might want to:
Quote:
Originally Posted by wyldckat View Post
try contacting OpenCFD's support http://www.openfoam.com/support/ - at the very least, they can give you a straight answer if this can be simulated with the current version of OpenFOAM and how much it would cost to implement this is, in case it doesn't have this feature yet.
Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   April 20, 2014, 11:18
Default
  #6
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,020
Blog Entries: 39
Rep Power: 109
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
Hi Ovie,

I finally managed to give a look into this. Just to be clear, I'm not an expert on this, but I believe that you can't use a constant alpha angle, given that it oscillates that much.

You'll need to search more about this, but the "dynamicAlphaContactAngle" seems to be what you should be using for the walls. For example (a somewhat bad one I tried):
Code:
    walls
    {
        type           dynamicAlphaContactAngle;
        theta0         45;
        uTheta         10;
        thetaA         10;
        thetaR         60;
        limit          gradient;
        value          uniform 0;
    }
For the meaning of each variable, the source code at "$FOAM_SRC/transportModels/twoPhaseProperties/alphaContactAngle/dynamicAlphaContactAngle/dynamicAlphaContactAngleFvPatchScalarField.H" has these comments:
Code:
        //- Equilibrium contact angle
        scalar theta0_;

        //- Dynamic contact angle velocity scale
        scalar uTheta_;

        //- Limiting advancing contact angle
        scalar thetaA_;

        //- Limiting receeding contact angle
        scalar thetaR_;
Best regards,
Bruno
__________________
wyldckat is offline   Reply With Quote

Old   April 21, 2014, 16:17
Default
  #7
Member
 
Ovie Doro
Join Date: Jul 2009
Posts: 99
Rep Power: 10
ovie is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
Hi Ovie,

I finally managed to give a look into this. Just to be clear, I'm not an expert on this, but I believe that you can't use a constant alpha angle, given that it oscillates that much.

You'll need to search more about this, but the "dynamicAlphaContactAngle" seems to be what you should be using for the walls. For example (a somewhat bad one I tried):
Code:
    walls
    {
        type           dynamicAlphaContactAngle;
        theta0         45;
        uTheta         10;
        thetaA         10;
        thetaR         60;
        limit          gradient;
        value          uniform 0;
    }
For the meaning of each variable, the source code at "$FOAM_SRC/transportModels/twoPhaseProperties/alphaContactAngle/dynamicAlphaContactAngle/dynamicAlphaContactAngleFvPatchScalarField.H" has these comments:
Code:
        //- Equilibrium contact angle
        scalar theta0_;

        //- Dynamic contact angle velocity scale
        scalar uTheta_;

        //- Limiting advancing contact angle
        scalar thetaA_;

        //- Limiting receeding contact angle
        scalar thetaR_;
Best regards,
Bruno
Hi Bruno:

Thanks for looking into this. I would implement the dynamic contact angle BC and let you know the results.

Thanks again!
ovie is offline   Reply With Quote

Old   April 21, 2014, 16:37
Default
  #8
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,020
Blog Entries: 39
Rep Power: 109
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
Hi Ovie,

I forgot to mention that you might need to do some more research on this topic, as implied by this paper: Impacting droplets: dynamic contact angle modelling in OpenFOAMŪ - this paper indicates that another model had to be implemented by the paper's authors in order to better simulate the following:
Quote:
The spreading and receding behavior of simulated water droplets impacting onto automobile wind shields or aircraft wings is not only determined by their initial conditions, but also influenced by the evolution of the contact angle throughout the impact scenario.
In your case, it's sort of the opposite and yet the same: although the droplet is meant to be stuck in the same place, the initial condition makes it wobble and leads to the observed motion. If the wobbling was better contained by the contact angle model, then it might not move.

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   April 21, 2014, 16:55
Default
  #9
Member
 
Ovie Doro
Join Date: Jul 2009
Posts: 99
Rep Power: 10
ovie is on a distinguished road
Great! Thanks!
ovie is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
interFoam vs. simpleFoam channel flow comparison DanM OpenFOAM Running, Solving & CFD 11 January 5, 2013 07:21


All times are GMT -4. The time now is 09:37.